OpenFOAM-dev / data /src /finiteVolume /fields /fvPatchFields /derived /flowRateInletVelocity /flowRateInletVelocityFvPatchVectorField.H
| /*---------------------------------------------------------------------------*\ | |
| ========= | | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | |
| \\ / O peration | Website: https://openfoam.org | |
| \\ / A nd | Copyright (C) 2011-2026 OpenFOAM Foundation | |
| \\/ M anipulation | | |
| ------------------------------------------------------------------------------- | |
| License | |
| This file is part of OpenFOAM. | |
| OpenFOAM is free software: you can redistribute it and/or modify it | |
| under the terms of the GNU General Public License as published by | |
| the Free Software Foundation, either version 3 of the License, or | |
| (at your option) any later version. | |
| OpenFOAM is distributed in the hope that it will be useful, but WITHOUT | |
| ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or | |
| FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License | |
| for more details. | |
| You should have received a copy of the GNU General Public License | |
| along with OpenFOAM. If not, see <http://www.gnu.org/licenses/>. | |
| Class | |
| Foam::flowRateInletVelocityFvPatchVectorField | |
| Description | |
| Velocity inlet boundary condition creating a velocity field with | |
| optionally specified profile normal to the patch adjusted to match the | |
| specified mass flow rate, volumetric flow rate or mean velocity. | |
| For a mass-based flux: | |
| - the flow rate should be provided in kg/s | |
| - if \c rho is "none" the flow rate is in m3/s | |
| - otherwise \c rho should correspond to the name of the density field | |
| - if the density field cannot be found in the database, the user must | |
| specify the inlet density using the \c rhoInlet entry | |
| For a volumetric-based flux: | |
| - the flow rate is in m3/s | |
| Usage | |
| \table | |
| Property | Description | Required | Default value | |
| massFlowRate | Mass flow rate [kg/s] | no | | |
| volumetricFlowRate | Volumetric flow rate [m^3/s] | no | | |
| meanVelocity | Mean velocity [m/s] | no | | |
| profile | Velocity profile | no | | |
| rho | Density field name | no | rho | |
| rhoInlet | Inlet density | no | | |
| alpha | Volume fraction field name | no | | |
| \endtable | |
| Example of the boundary condition specification for a volumetric flow rate: | |
| \verbatim | |
| <patchName> | |
| { | |
| type flowRateInletVelocity; | |
| volumetricFlowRate 0.2; | |
| profile laminarBL; | |
| } | |
| \endverbatim | |
| Example of the boundary condition specification for a mass flow rate: | |
| \verbatim | |
| <patchName> | |
| { | |
| type flowRateInletVelocity; | |
| massFlowRate 0.2; | |
| profile turbulentBL; | |
| rho rho; | |
| rhoInlet 1.0; | |
| } | |
| \endverbatim | |
| Example of the boundary condition specification for a mean velocity: | |
| \verbatim | |
| <patchName> | |
| { | |
| type flowRateInletVelocity; | |
| meanVelocity 5; | |
| profile turbulentBL; | |
| } | |
| \endverbatim | |
| The \c volumetricFlowRate, \c massFlowRate or \c meanVelocity entries are | |
| \c Function1 of time, see Foam::Function1s. | |
| The \c profile entry is a \c Function1 of the normalised distance to the | |
| wall. Any suitable Foam::Function1s can be used including | |
| Foam::Function1s::codedFunction1 but Foam::Function1s::laminarBL and | |
| Foam::Function1s::turbulentBL have been created specifically for this | |
| purpose and are likely to be appropriate for most cases. | |
| Note: | |
| - \c rhoInlet is required for the case of a mass flow rate, where the | |
| density field is not available at start-up | |
| - The value is positive into the domain (as an inlet) | |
| - May not work correctly for transonic inlets | |
| - Strange behaviour with potentialFoam since the U equation is not solved | |
| See also | |
| Foam::fixedValueFvPatchField | |
| Foam::Function1s::laminarBL | |
| Foam::Function1s::turbulentBL | |
| Foam::Function1s | |
| Foam::flowRateOutletVelocityFvPatchVectorField | |
| SourceFiles | |
| flowRateInletVelocityFvPatchVectorField.C | |
| \*---------------------------------------------------------------------------*/ | |
| // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // | |
| namespace Foam | |
| { | |
| /*---------------------------------------------------------------------------*\ | |
| Class flowRateInletVelocityFvPatchVectorField Declaration | |
| \*---------------------------------------------------------------------------*/ | |
| class flowRateInletVelocityFvPatchVectorField | |
| : | |
| public fixedValueFvPatchVectorField | |
| { | |
| // Private Data | |
| //- Inlet integral flow rate | |
| autoPtr<Function1<scalar>> flowRate_; | |
| //- Is the flow-rate mean velocity? | |
| bool meanVelocity_; | |
| //- Is the flow-rate volumetric? | |
| bool volumetric_; | |
| //- Optional velocity profile | |
| autoPtr<Function1<scalar>> profile_; | |
| //- Name of the density field used to normalise the mass flux | |
| word rhoName_; | |
| //- Rho initialisation value (for start; if value not supplied) | |
| scalar rhoInlet_; | |
| //- Name of the volume fraction field used to convert to interstitial | |
| // velocity | |
| word alphaName_; | |
| //- Normalised distance to the wall | |
| scalarField y_; | |
| //- Total area of patch | |
| scalar area_; | |
| // Private Member Functions | |
| //- Set the wall distance field y_ | |
| void setWallDist(); | |
| //- Return the normalised velocity profile | |
| virtual tmp<scalarField> profile(); | |
| //- Update the patch values given the appropriate volume fraction and | |
| // density types and values | |
| template<class ScaleType, class AlphaType, class RhoType> | |
| void updateValues | |
| ( | |
| const ScaleType& scale, | |
| const AlphaType& alpha, | |
| const RhoType& rho | |
| ); | |
| //- Update the patch values given the appropriate volume fraction type | |
| // and values | |
| template<class AlphaType> | |
| void updateValues(const AlphaType& alpha); | |
| public: | |
| //- Runtime type information | |
| TypeName("flowRateInletVelocity"); | |
| // Constructors | |
| //- Construct from patch, internal field and dictionary | |
| flowRateInletVelocityFvPatchVectorField | |
| ( | |
| const fvPatch&, | |
| const DimensionedField<vector, fvMesh>&, | |
| const dictionary& | |
| ); | |
| //- Construct by mapping given | |
| // flowRateInletVelocityFvPatchVectorField | |
| // onto a new patch | |
| flowRateInletVelocityFvPatchVectorField | |
| ( | |
| const flowRateInletVelocityFvPatchVectorField&, | |
| const fvPatch&, | |
| const DimensionedField<vector, fvMesh>&, | |
| const fieldMapper& | |
| ); | |
| //- Disallow copy without setting internal field reference | |
| flowRateInletVelocityFvPatchVectorField | |
| ( | |
| const flowRateInletVelocityFvPatchVectorField& | |
| ) = delete; | |
| //- Copy constructor setting internal field reference | |
| flowRateInletVelocityFvPatchVectorField | |
| ( | |
| const flowRateInletVelocityFvPatchVectorField&, | |
| const DimensionedField<vector, fvMesh>& | |
| ); | |
| //- Construct and return a clone setting internal field reference | |
| virtual tmp<fvPatchVectorField> clone | |
| ( | |
| const DimensionedField<vector, fvMesh>& iF | |
| ) const | |
| { | |
| return tmp<fvPatchVectorField> | |
| ( | |
| new flowRateInletVelocityFvPatchVectorField(*this, iF) | |
| ); | |
| } | |
| // Member Functions | |
| // Mapping functions | |
| //- Map the given fvPatchField onto this fvPatchField | |
| virtual void map(const fvPatchVectorField&, const fieldMapper&); | |
| //- Reset the fvPatchField to the given fvPatchField | |
| // Used for mesh to mesh mapping | |
| virtual void reset(const fvPatchVectorField&); | |
| // Evaluation functions | |
| //- Update the coefficients associated with the patch field | |
| virtual void updateCoeffs(); | |
| // I-O | |
| //- Write | |
| virtual void write(Ostream&) const; | |
| // Member Operators | |
| //- Inherit assignment | |
| using fixedValueFvPatchVectorField::operator=; | |
| }; | |
| // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // | |
| } // End namespace Foam | |
| // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // | |
| // ************************************************************************* // | |